Deviation from round when milling a circular boss

[dbb-the-bruce]

Not really looking for answers here, just an observation and interested in comments.

Still getting to know my Tormach 770M. I had to make some small parts - a round base ~.500 dia with other features milled on one end. Pre-CNC, I would have turned the boss / round on my lathe and then held the part by the round end in a vise on my bench mill. I figured this would be a good opportunity to make a soft / AL jaw set for my fixture plate. One op to hold the raw bar stock and mill the final boss/round, flip over and do the non-round milling all on the CNC.

The round needs to fit pretty precisely in the hole it will end up in so I was trying to get the diameter as close as possible. I did a finish cut leaving .005 radial with the intention of then being able to measure and take one last cut to hit the target diameter.

In the process, I discovered that the diameters of the parts (I was making two, exact same model and tool parts for each) seemed to be off by .0015
Now let me be clear here - that's close enough for what I'm doing, but these are two identical circular bosses cut with the same brand new end mill on a very new machine.

When I finished them up and could pull them out of the soft jaws, I was able to take better measurements and determined that they were in fact damn near identical, they just happened to be not quite round! Back to my original motivation - I knew at the start that If I wanted perfect cylindrical parts for a tight fit in a reamed hole, that I'd be better off doing that on my lathe.

However, considering the extra milling on the other end of the part, they are also a good use of a CNC machine - just hold the round end and all the other steps can be done in one fixture rather than the fussing around it takes to do it on my manual mill.

So my experiment confirmed my suspicions - (maybe). I can get < .0005 error on small round parts on my lathe. Getting .0015 diameter error on a small round part on my CNC machine is acceptable as long as I'm aware of it (and if the actual required tolerance / fit is anywhere near that).

Just for fun, I drew up a diagram that exaggerates the error of 4 diameters I measured on both parts:

View attachment 512044
I'm guessing the error comes from either machine wind-up (lead screws), controller tracking (stepper motors) or backlash.
Interestingly the error is greater in the Y axis - which implies the physics of the machine are involved. I did a bunch of work with ultra-high precision XY stages for positioning micro-chips during lithography. Because the Y stage (typically) carries the X stage, it has significantly more mass (+2X) and hence is noticeably harder to accelerate.

Hope you found this interesting.

Finish cut was using a 3/8 3 Flute carbide end mill, 4000 RPM, 10 in/min
very slow.
Do you think I could get it more accurate? other than buying one of those really cool lath mill combo machines!

 

[dbb-the-bruce]

Sorry about the duplicate post - something wacky happened when I tried to make minor edits...

 

[682bear]

My guess... it's caused by play in the screws. It's more noticeable in the Y axis because the Y screw has more play. If it is caused by wear, that would make sense... the Y axis screw has to carry more weight, so would wear faster.

The CNC VTLs that I run at work are laser calibrated every year... the calibration measures the backlash, which is then entered into a machine parameter setting. This is supposed to automatically adjust out the backlash every time the screws are reversed... it never works out entirely accurately, probably because different areas of the screws have different amounts of wear.

-Bear

 

[Eddyde]

Sorry about the duplicate post - something wacky happened when I tried to make minor edits...

Sorry, I deleted the first post thinking this was an exact duplicate.

 

[dbb-the-bruce]

Sorry, I deleted the first post thinking this was an exact duplicate.

Ha! no problem. I was looking for a way to delete it, I guess we can't do that. What's weird now is when I click edit I get a blank input box. That's kind of what happened when I first tried to edit.

 

[dbb-the-bruce]

Back to the parts at hand -
I've been contemplating them while drinking coffee (actually I just like to fidget with stuff), and I noticed that there is a perceptible bump at the Y axis extremes - the direction change. It's funny how you can feel something like that that you can't even see. The "bumps" are less than .001 more like .0005

Anyhow, I decided to take more diameters and sure enough, most of them are the same until you get a few degrees off of Y min/max. Then the diameter bumps up a little more than a .001. Without going crazy, it would be hard to be more accurate - and I don't care.

I think that this is more indicative of backlash at the Y turn around.

 

[RJSakowski]

When I bought my 770 Series 3 mill, I asked the salesman why I needed a boring head when I could use a pocketing routine. His answer was that a CNC won't cut a truly round hole with a pocketing routine due to what they term as lost motion. Lost motion causes a small glitch whenever the direction of the cut reverses which is at the four compass points. Here is an exaggerated depiction of the errors caused by lost motion when using a pocketing routine using a .250" end mill. The blue circle show the largest inscribed circle which is smaller in diameter than the nominal circle by about the amount of lost motion.


Lost motion is a combination of backlash and torque windup. Backlash on the 770 is due to insufficient thrust bearing preload and/or ball screw nut preload. You can't do anything about the ball nut short of rebuilding it. Play is usually addressed by replacing the existing balls with very slightly larger ones.

The thrust bearing preload is adjustable. The Tormach procedure consists of measuring backlash while increasing the preload. When the preload starts to increase, you back the adjustment off slightly and lock it. I prefer to measure torque required to turn the ball screw and lock it as it just starts to rise. There will be about a thousandth of lost motion.

When cutting a pocket or boss that has to have tight tolerances, I purposely set my tool diameter slightly larger than nominal which will result in a slightly smaller hole or larger boss. Then I measure and/or check my fit and make appropriate adjustments to the tool diameter to achieve the desired result. (This is easier than modifying the G code). If one wished to have a smoother pocket, the cut could be run as both a climb cut and a conventional cut. This will eliminate the jogs at the quadrants and a pin that is smaller by about 1/2 the lost motion will fit the resultant pocket.

 

[400bird]

Funny thing, my 1980's CNC knee mill also does the same thing and now it makes sense. But to a much greater extent, it's visible by eye. Prob about 1mm for each of the 4 bump outs in lost movement. I think I've got a preload issue on the ball screw bearings, I just need to find it.